[musa19]

Hi,
I'm trying to run a case in cfx, but the problem was reported:

* ERROR # 002100012 has occurred in subroutine cVolSec. |
* | Message: |
* | A negative ELEMENT volume Has Been detected. This is a fatal |
* | Error and execution will be terminated. The location of the first |
* | Reported negative volume is below. |

But I checked ICEM meshing and I did not find any negative volume cells. I did run for problems, I find some single elements. I am attaching the pictures.

Kindly help me why I am getting negative volume, and how can I fix it. Thank you.

[ghorrocks]

The error message does not lie; you really do have an inside-out element. It should report the XYZ location of it so you can find it.

If this occurs at the start of your simulation then the mesh you generated is the problem.

If this occurs a while into a moving mesh simulation then the way you are moving the mesh does not work.

Here are some more tips: https://www.cfd-online.com/Wiki/Ansy..._went_wrong.3F

[Gert-Jan]

Sure your mesh needs some improvements.
Nevertheless, I have had a similar case, where I got these messages appearing in double precision mode, and not in single precision. Do you run in double precision?
And in another case I got the messages after translation of my mesh in Pre. There, ICEM thought everything was OK, whereas Pre lost accuracy, resulting in an error in subroutine cVolSec. So did you translate/rotate the mesh in Pre?

[musa19]

Thank you Glenn and Gert for your precious time. Firstly, I checked the mesh in ICEM quality and it shows no negative element.
Yes I am doing PITCHING AIRFOIL CASE/moving mesh study. I am getting this error after few iterations.

I tried in double precision, but I will try it in single precision as well.

Your help is highly appreciated. How should I solve this issue. Thank you.

[Gert-Jan]

You can look in ICEM as long as you like, but you won't find the problem nor solution there. It definitely has to do with moving/deforming mesh.
I expect you have to reduce timestep or alter the settings of the mesh deformation to prevent CFX from creating a negative volumue.

Good luck. You might need that.

Regs, Gert-Jan

[musa19]

Hi Glenn, thank you for your time. My time step is 0.00003. It is already small. I will look into it why it is creating the problem.
In the mean time, if you have any suggestions, please let me know. Thank you.

[ghorrocks]

Your time step is unlikely to have anything to do with the problem. What is likely to be happening is the mesh is folding as it moves. Have you read the FAQ I linked to? https://www.cfd-online.com/Wiki/Ansy..._went_wrong.3F

[musa19]

Hi Glenn and Gert,
Thank you for your seggestions. I was able to figure out the issue. It was bascically the trailing edge mesh. I changed the trailing edge from blunt to round and it worked.
I need help in plotting hystersis loops for lift and drag in CFX. How can I obtain the loops in CFX. I have attached two pictures as an example. Your help is highly appreciated.

Thank you.

[ghorrocks]

I hope you are not using moving mesh to get these AOA curves. Talk about doing it the hard way.....

[musa19]

Hi Glenn,
Thank you for your reply. I am doing transient analysis on an oscillating airfoil using Mesh deformation with regions of motion specified in CFX. I use expressions for lift and drag but they provide results for a particular alpha only. I want to plot the hystersis loop for pitching airfoil.
Can you guide me accordingly. Thank you.

[ghorrocks]

If you are just looking for the lift and drag curve then you should do this using fixed mesh simulations with the AOA adjusted for each simulation.

If your intention is to model transient behaviour of an oscillating airfoil, then the easiest way to do it is if you can model this with the lift and drag curve from fixed mesh models then a ODE solver to model the motion. This only works if the transient motion does not affect the lift or drag based on the speed you are modelling. In other words, you can assume a separation of time scales - the flow time scale is fast compared to the motion time scale.

If you cannot assume a separation of time scales and the transient motion does affect the lift and drag (which your comment that you want the hysteresis would imply) then you have to model this with a transient mesh deformation simulation.

If you are getting negative volume elements in a moving mesh simulation I recommend you read the FAQ (https://www.cfd-online.com/Wiki/Ansy..._went_wrong.3F) and adjust the mesh deformation diffusion as it suggests. Use the techniques describes to debug this problem quickly.